Master’s Thesis 2018 30 ECTS
Faculty of Science and Technology (REALTEK) Themistoklis Tsalkatidis
Parametric study of an aluminium K-joint
Trym Hauge Nilsen
Civil engineering and architecture
Faculty of Science and Technology (REALTEK)
1
2
Preface
This master thesis marks the end of my five years education – Civil engineering and architecture at the Norwegian University of Life Science (NMBU).
The topic of this master thesis was selected in collaboration with associate professor Themistoklis Tsalkatidis, who also was my thesis supervisor. The reason for selecting this topic was my interest in Aluminium and my wish to learn more about a material that has not been of high priority in prior years of my education. I have also good experiences with FEM programming and numerical analyses was a natural way to investigate the selected structure.
The work has been time consuming and the learning curve was steep throughout the project. It has given me more experience in FEM programming, especially in software program ANSYS, and I have learned much about aluminium as a material. This experience is something I will bring with me in future years.
I would like to thank my supervisor associate professor Themistoklis Tsalkatidis for his guidance and interest during the writing and modelling of this theses. Especially his positivity and motivation when challenges were encountered.
I would also like to thank my classmates for a good environment to work in. A special thanks to Sonja Helene Servan, Synne Lofthus Rooth and Tord Hauge Nilsen for looking critically through my work and helping me make the thesis better. Finally, I would like to thank my family and friends for encouragement and support during the spring.
3
4
Abstract
Aluminium is a construction material which has increased in use over the past 50 years. Its low weight makes it preferable in portable structures. K-joint is the main joint in trusses and these trusses are used in scaffolds and moveable stages where large spans are present. Although some research has been done during the last 20 years, there is still a lot of potential to make more studies of aluminium structures. In this thesis, numerical models of a K-joint made from CHS profiles have been made based on the experimental data in Đuričić et al. (2017). It is parametric studies where brace angle and chord thickness, and their influence on deformation and resistance, have been investigated. Since there is no direct approach described to calculate resistance in aluminium K-joints, it has also been investigated if the steel theory in EN1993-1- 8 (2005) sufficiently describes the behaviour of the models created.
Four case studies were modelled in FEM program ANSYS. A reference model with brace angle 45˚ and chord thickness of 2 mm was made and validated with the experimental results in Đuričić et al. (2017). Two models with brace angle 30˚ and 60˚ were created to study the effect of brace angle changes. To investigate the chord thickness, a model where the chord thickness was increased from 2 mm to 3 mm was made. All the models were loaded at the compressed brace member, the resulting deformations and von mises stresses were investigated. Strength of the models is found with the deformation limits described by Lu et al. (1994). The strengths are compared to each other to investigate the influence of the different parameters. Design resistances are calculated based on the steel theory in EN1993-1-8(2005), with the addition of aluminium softening described in EN1999-1-1(2007). These calculations are compared to the numerically obtained strengths, in order to investigate the corralation between them.
The numerical results experience a 20 % increase of the design strength against chord plastification as the brace angle is decreased from 45˚ to 30˚ and an increase of 5 % when the angle is changed from 60˚ to 45˚. The model with increased chord thickness experiences a different failure mode than the other models. The braces fail from stresses in the heat affected zones exeeding the ultimate strength.
Hand calculation results show a good correlation with the model with low brace angle. It gives very conserative values for the K-joints with larger brace angles. The K-joint with chord thickness 3 mm is not sufficiently described by the steel theory since axial failure in the braces needs to be considered in addition to the chord plastification failure.
5
6
Sammendrag
Bruken av aluminium som et konstruksjonsmateriale har økt over de siste 50 årene. Den lave vekten gjør det foretrukket i midlertidige konstruksjoner. K-forbindelser er hovedkomponenten i fagverk som brukes i stillas og midlertidige scener hvor store spenn er tilstede. Det er gjort noen studier på denne typen forbindelser de siste 20 årene, men det er fortsatt stort potensial til å forske mer på dette. I denne oppgaven er det laget numeriske modeller av K-forbindelser laget av CHS profiler basert på eksperimentelle data i Đuričić et al. (2017). Det er en parametrisk studie hvor stegstavenes vinkel og tykkelsen på gurtstaven, og deres innvirkning på deformasjon og styrke, har blitt undersøkt. Siden det ikke finnes en direkte metode for å beregne styrke i aluminium K-forbindelser, har det også blitt undersøkt om stålteorien i EN1993-1-8 (2005) beskriver oppførselen til modellene tilstrekkelig.
Fire strukturer har blitt modelert i FEM programmet ANSYS. En referansemodell med stegvinkel på 45˚ og gurtstavtykkelse på 2 mm har blitt laget og validert opp mot de eksperimentelle resultatene i Đuričić et al. (2017). To modeller med stegvinkel på 30˚ og 60˚
er bygget for å studere effekten av endringer av vinkelen. For å undersøke gurttykkelsen ble det modellert en K-forbindelse med økt gurttykkelse fra 2 mm til 3 mm. Alle modellene var lastet på stegstaven som var i trykk, resulterende deformasjoner og von mises spenninger ble undersøkt. Styrken til modellene er funnet med deformasjonsgrensene beskrevet av Lu et al.
(1994). Styrkene er sammenlignet for å undersøke påvirkningen av de forskjellige parametrene.
Dimensjonerende styrke er beregnet basert på stålteorien i EN1993-1-8 (2005), med innvirkning av oppmykning i aluminium beskrevet i EN1999-1-1 (2007). Disse beregningene er sammenliknet med de numeriske styrkene for å undersøke sammenhengen mellom dem.
De numeriske resultatene opplever en økning av styrken mot flensbrudd i gurten på 20 % når stegvinkelen endres fra 45˚ til 30˚ og en økning på 5 % når vinkelen endres fra 60˚ til 45˚.
Modellen med økt gurttykkelse opplever en annen bruddform enn de andre modellene.
Stegstavene går i brudd fra de aksielle spenningene i de varmepåvirkede sonene som overstiger bruddspenningene.
Håndberegningene gir god korrelasjon med modellen med liten stegvinkel. De gir veldig konservative verdier for K-forbindelsene med større stegvinkler. Forbindelsen med gurttykkelse på 3 mm er ikke tilstrekkelig beskrevet av stålteorien siden aksielt brudd i stegene må vurderes i tillegg til flensbrudd i gurten.
7
8
Table of content
Preface ... 2
Abstract ... 4
Sammendrag ... 6
List of figures ... 12
List of tables ... 13
List of symbols ... 14
1 Introduction ... 16
1.1 Background ... 16
1.2 Objective ... 16
2 Theory ... 18
2.1 Material ... 18
2.1.1 History and use of aluminium ... 18
2.1.2 Numbering and temper designations of aluminium alloys ... 18
2.1.3 Aluminium alloy EN AW-6082 T6 ... 20
2.1.4 Heat-affected zone ... 21
2.2 Stress-strain relationship ... 22
2.3 Design of K-joints ... 25
2.3.1 Failure modes ... 25
2.3.2 Design axial resistances for K-joints ... 27
2.3.3 Aluminium softening reduction factor ... 29
2.4 Previous analysis of k-joints ... 30
2.5 The finite element method ... 31
2.5.1 Boundary conditions and loading ... 33
2.5.2 Linear analysis ... 33
2.5.3 Nonlinear analysis ... 33
2.6 ANSYS Mechanical APDL ... 34
9
2.6.1 Element type used in ANSYS ... 34
2.6.2 Element size and Meshing ... 35
2.6.3 Multilinear isotropic hardening (TB,MISO) ... 35
3 Methodology ... 36
3.1 Introduction ... 36
3.2 Different K-joints to be modelled ... 36
3.3 Numerical analysis ... 37
3.3.1 Geometry ... 37
3.3.2 Element selection and meshing ... 38
3.3.3 Material input ... 39
3.3.4 Stress-strain curves ... 40
3.3.5 Boundary conditions and loads ... 43
3.3.6 Analysis type and postprocessing ... 44
3.5 Hand calculations of K-joint ... 45
3.5.1 Calculations without consideration of heat affected zone ... 45
3.5.2 Calculations with consideration of heat affected zone ... 46
3.5.3 Comparison of numerical results and hand calculations ... 47
4 Results ... 48
4.1 Numerical analysis ... 48
4.2 Hand calculations ... 54
4.3 Comparison of Numerical results and hand calculations ... 55
5 Discussion ... 58
5.1 Modelling process ... 58
5.2 Validation of the model ... 58
5.3 Interpretation of numerical results of parametric study ... 59
5.3.1 Difference in brace angle ... 59
5.3.2 Increased thickness of chord member ... 59
10
5.4 Comparison of hand calculated results and numerical results ... 60
5.4.1 Different brace angles ... 60
5.4.2 Different thickness of chord ... 61
6 Conclusion ... 62
7 Recommended for future work ... 64
8 References ... 66
Annex A ... 68
Annex B ... 72
Annex C ... 74
11
12
List of figures
Figure 1: Bi-linear model (left) and three-linear model (right) of stress-strain relationship
(EN1999-1-1, 2007) ... 24
Figure 2: Failure modes for jonts made of CHS-profiles (EN1993-1-8, 2005) ... 26
Figure 3: Gap K-joint with geometric sizes (EN1993-1-8, 2005) ... 27
Figure 4: Logical diagram of the process of finite element analysis(Bathe, 2006)... 32
Figure 5: Geometry of SOLID285 element (ANSYS, version 18.2, Academic) ... 35
Figure 6: Geometry of investigated models ... 37
Figure 7: Initial model of k-joint with angle of 45 degrees... 38
Figure 8: Mesh of k-joint ... 39
Figure 9: Plot of Ø50x2 mm stress-strain curve ... 41
Figure 10: Plot of Ø20x2 mm stress-strain curve ... 41
Figure 11: Plot of HAZ1 stress-strain curve ... 42
Figure 12: Plot of HAZ2 stress-strain curve ... 43
Figure 13: Structure with applied boundary conditions and loading ... 43
Figure 14: Extent of heat affected zone(Đuričić et al., 2017) ... 46
Figure 15: Deformed shape of model 1 ... 48
Figure 16: Force-deformation of model 1 ... 48
Figure 17: Countur plot of von mises stress in HAZ1 of model 1 ... 49
Figure 18: Deformed shape of model 2 ... 50
Figure 19: Force-deformation of model 2 ... 50
Figure 20: Deformed shape of model 3 ... 51
Figure 21: Force-deformation of model 3 ... 51
Figure 22: Deformed shape of model 4 ... 52
Figure 23: Plot of force-deformation for model 4 ... 52
Figure 24: Contour plot of von mises stress in HAZ1 of model 4 ... 53
Figure 25: Combined force-deformation graph for all models ... 53
Figure 26: Joint resistances for different angled k-joints ... 55
13
List of tables
Table 1: Numerical designation system for wrought aluminium alloys (Müller, 2011) ... 19
Table 2: Basic temper designation (Müller, 2011) ... 20
Table 3: Chemical composition of EN AW-6082, in %, rest is aluminium (EN573-3, 2013) 20 Table 4: Mechanical properties of EN AW-6082 T6 (EN755-2, 2016) ... 20
Table 5: Engineering stress-strain relations (Đuričić et al., 2017) ... 21
Table 6: Stresses of material in HAZs (Heat affected zones) (Đuričić et al., 2017) ... 22
Table 7: Validity range for welded joints between CHS brace members and CHS chords (EN1993-1-8, 2005) ... 27
Table 8: Different models to investigate ... 36
Table 9: True stresses in CHS profile ... 39
Table 10: Stresses for heat affected zones ... 40
Table 11: Multilinear isotropic hardening table for Ø50x2 mm in ANSYS ... 40
Table 12: Multilinear isotropic hardening table for Ø20x2 mm in ANSYS ... 41
Table 13: Multilinear isotropic hardening table for HAZ1 in ANSYS ... 42
Table 14: Multilinear isotropic hardening table for HAZ2 in ANSYS ... 42
Table 15: Pressure applied on compressed brace ... 44
Table 16: Calculations according to Eurocode 3 part 1-8 ... 45
Table 17: Calculation of design resistance of softened cross-section ... 47
Table 18: Results of hand calculations for model 1 ... 54
Table 19: Results of hand calculations for model 2 ... 54
Table 20: Results of hand calculations for model 3 ... 54
Table 21: Results of all hand calculations for model 4 ... 55
Table 22: Relation between numerical results and hand calculations ... 56
Table 23: Relation between different angled connections ... 56
14
List of symbols
Δ𝑢 - ultimate strength deformation limit Δ𝑠 - serviceability strength limit
𝛾 - ratio of brace member diameter to twice its wall thickness 𝛾𝑀5 - partial safety factor for resistance of joints
𝜀 - strain
𝜀𝑒 - strain corresponding to 𝑓𝑒 𝜀𝑒𝑛𝑔 - engineering strain 𝜀𝑝 - strain corresponding to 𝑓𝑝 𝜀𝑚𝑎𝑥 - strain corresponding to 𝑓𝑚𝑎𝑥
𝜃𝑖 - angle between brace member i and chord member 𝜌0,ℎ𝑎𝑧 - strength reduction factor for heat affected zone 𝜎 - stress
𝜎𝑒𝑛𝑔 - engineering stress
A - elongation measured over a gauge length of 5.65√𝑆0 (where 𝑆0 is the initial cross-sectional area of the test piece)
A50mm - elongation measured over a gauge length of 50 mm 𝑑𝑖 - diameter of brace member i
𝑑0 - diameter of chord E - elastic modulus
𝐸1 - first hardening modulus 𝐸2 - second hardening modulus 𝑓0 - 0,2% proof strength
𝑓1% - 1% tensile strength 𝑓3% - 3% tensile strength 𝑓𝑢 – ultimate tensile strength
𝑓0,𝐻𝐴𝑍 - 0,2% proof strength of heat affected zone 𝑓𝑢,𝐻𝐴𝑍 - ultimate tensile strength of heat affected zone 𝑓𝑝 - elastic limit of proportionality
𝑓𝑚𝑎𝑥 - maximum stress in stress-strain diagram 𝑓𝑒 - limit of elasticity
15 𝑓𝑦0 - yield strength of chord
𝑔 - gap between brace members HB - Brinell hardness
HV - Vickers hardness 𝑲 - stiffness matrix
𝑘𝑔 - k-joint geometry factor 𝑘𝑝 - chord stress factor
𝑘𝑎𝑙 - aluminium softening reduction factor 𝐿∗ - arc length of softening zone
L - circumference of chord member cross section 𝑁𝑖,𝑅𝑑 - resistance force in brace member i
𝑁𝑢 - ultimate strength 𝑁𝑠 - serviceability strength R – load vector
𝑅𝑝0,2 - yield stress 𝑅𝑚 - tensile strength
𝑡𝑖 - thickness of brace member i 𝑡0 - thickness of chord
U - displacement vector
16
1 Introduction
1.1 Background
Aluminium is a light material, this reduces the cost of transportation, work and assembly since less resources are needed to transfer the elements. Another advantage is the ease of recycling aluminium, since only 5% of the energy required for primary production is used for recycling.
This can help achieve the norms on sustainability and recyclability in the construction industry, to limit the impact on the environment in the manufacturing and building process. The use of aluminium as a construction material has increased, therefore a Eurocode solely about aluminium was created. Eurocode 9 establishes design criteria for this material (Müller, 2011).
There are some disadvantages of aluminium as well. The modulus of elasticity is about one third that of steel, the level of heat conductivity is high and the production cost is high (Đuričić et al., 2017).
K-joints are the main components of truss elements. Trusses are used for large spans and aluminium trusses are often used for stage elements, scaffolds and other transportable structures where the decrease of weight is of importance. They consist of chords and braces welded together and these are mainly loaded by axial compression or tension forces (Đuričić et al., 2017).
Circular hollow sections (CHS) have excellent properties in resisting compression, tension, bending and torsion. Related to other elements, CHS have a favourable shape when being subjected to loading. With these good characteristics, open designs can be made allowing an architecturally attractive shape of elements (Wardenier et al., 2008).
1.2 Objective
Various shapes and sizes of aluminium trusses can create many different brace angles in the K- joints. This is a parametric study of a K-joint made from circular hollow sections (CHS) in aluminium alloy EN AW-6082 T6. The primary objective is to investigate the effect of changing brace angle and thickness of the chord, with focus on how this influences deformation
17
and resistance of the connection. While K-joints made from steel have been studied extensively, similar joints made from aluminium have been less investigated. The most common approach for designing K-joints of aluminium CHS profiles is to use the same theory as for steel joints.
Therefore, a secondary objective of this thesis is to investigate if the embracement of steel related theories sufficiently describes the behaviour of aluminium K-joints, especially their design resistance capacities. This will be investigated numerically by constructing three- dimensional models in ANSYS, a popular finite element program. Previous experiments on CHS K-joints in aluminium have been conducted by Đuričić et al. (2017) and the numerical models are created from the data in these experiments. The results from this study have been used to verify the numerical model.
18
2 Theory
2.1 Material
Aluminium has a density of approximately 2700 kg/m3, about one third of steel. It has a tensile strength of 90-140 N/mm2 and is classified as a weak metal. This means that for structural applications the aluminium must be strengthened. Strengthening is done by the method of alloying (Müller, 2011).
2.1.1 History and use of aluminium
Using aluminium alloys in structural engineering is quite new. While aluminium became possible to isolate in 1827, industrial production of aluminium did not start before 1886. Until the second world war, aluminium was only used for specific constructions, such as the aeronautical industry. It was not until after the second world war that the aluminium alloys started to be developed for use in civil engineering. The first building structures that consisted of aluminium alloys appeared as prefabricated systems in the early fifties in central Europe. At that time the absence of recommendations and codifications made the structural design difficult for engineers and controlling bodies. In Europe, this has been overcome first by the ECCS Recommendations issued in 1978 and up until now with the Eurocode 9 “Design of Aluminium Structures.” However, there is still much potential in these materials and further research must be performed (Mazzolani, 2012).
2.1.2 Numbering and temper designations of aluminium alloys
The main alloying elements create a base for numbering and incorporation within designated series. Currently the aluminium alloy designation for wrought aluminium is based on the system for alloy designation administered by the Aluminium Association Inc. The first digit in the alloy numbering relates to the series group, this is associated to the major alloying element used. The different series are presented in Table 1. If the alloys are Heat-treatable (HT) or non-heat- treatable (NHT) they are classified in different types (Müller, 2011).
19
Table 1: Numerical designation system for wrought aluminium alloys (Müller, 2011)
Series Alloying elements Type
1xxx None (aluminium 99% and greater) NHT
2xxx Copper (Cu) HT
3xxx Manganese (Mn) NHT
4xxx Silicon (Si) NHT
5xxx Magnesium (Mg) NHT
6xxx Magnesium and silicon (MgSi) HT
7xxx Zinc (Zn) HT
8xxx Other elements
If there is a modification from the specific alloy the second digit in the alloy numbering will be different from 0. The last two digits are there to identify the specific alloy in its series (Müller, 2011).
Due to the availability of different tempers, there is an additional mark for the aluminium alloy numbering. This temper designation and the resulting properties are dependent for the types of heat-treatable and non-heat-treatable alloys. For heat-treatable alloys, heat can be used to strengthen or soften the material, and heat is often used to help the forming process. To restore original properties, heat-treatable alloys can be re-heat-treated after the forming process is completed. For non-heat-treatable alloys, properties can only be improved by cold-working (Müller, 2011).
There are five basic designations used in the aluminium alloy temper designation system. For these five groupings the letters F, O, H, W and T is used. These letters represent different heat- treatments. The basic treatments are listed in Table 2 (Müller, 2011).
20
Table 2: Basic temper designation (Müller, 2011)
Letter Description Meaning
F As fabricated Forming process with no special control over thermal or strain hardening
O Annealed Heat treated to give min. strength improving ductility and dimensionality
H Strain hardened Strengthened by cold working
W Heat treated Solution heat treated but produces an unstable temper
T Heat treated Thermally heat treated with or without additional strain hardening
An additional number can be added to the temper designation to explain what type of treatment the alloy has been exposed to (Müller, 2011).
2.1.3 Aluminium alloy EN AW-6082 T6
The aluminium alloy EN AW-6082 T6 is a high strength alloy used mainly for highly loaded structurers. The 6000-series of aluminium alloys is much used for their favourable combination of mechanical properties. Alloy 6082 has a high strength after heat treatment as well as good corrosion resistance and good weldability (Wang et al., 2015). The temper T6 implies that the solution is heat treated, quenched and artificially aged (Müller, 2011). Table 3 and Table 4 gives chemical composition and mechanical properties of aluminium alloy EN AW-6082 T6.
Table 3: Chemical composition of EN AW-6082, in %, rest is aluminium (EN573-3, 2013)
Si Fe Cu Mn Mg Cr Zn Ti Others
Each Total 0,7-1,3 0,50 0,10 0,40-1,0 0,6-1,2 0,25 0,20 0,15 0,05 0,15
Table 4: Mechanical properties of EN AW-6082 T6 (EN755-2, 2016)
Wall thickness, t (mm)
Yield stress 𝑅𝑝0,2 (MPa)
Tensile strength 𝑅𝑚 (MPa)
Elongation Hardness
A HB (%)
A50mm (%)
≤ 5 5 < t ≤ 25
250 260
290 310
8 10
6 8
95 95
21
Experimental testing of CHS profiles made from alloy EN AW-6082 T6 was done by Đuričić et al. In this experiment 0,2 % proof strength (𝑓0), ultimate tensile strength (𝑓𝑢) and elongation for the material was investigated as well as two intermediate stresses (𝑓1%, 𝑓3%). This gave engineering stress values for Ø50x2 mm and Ø20x2 mm shown in Table 5 (Đuričić et al., 2017).
Table 5: Engineering stress-strain relations (Đuričić et al., 2017)
Profile(mm) 𝑓0(MPa) 𝑓1%(MPa) 𝑓3%(MPa) 𝑓𝑢(MPa) Elongation (%)
Ø50x2 309,34 333,69 339,42 342,48 5,56
Ø20x2 272,34 283,51 289,09 304,38 5,67
Elastic modulus for EN AW-6082 T6 is 69500 MPa (Đuričić et al., 2017).
2.1.4 Heat-affected zone
When welding aluminium alloy members, the generated heat will reduce the material properties near the welds. The yield strength in the heat affected zones is approximately one half of the original material yield strength and it is important to know the extent of heat-affected softening for design of a structure (Müller, 2011).
According to Eurocode 9 part 1-1, the heat-affected zone should be considered for the 6xxx- series in temper T4 and above. Eurocode 9 gives the characteristic values of 0,2 % proof strength (𝑓0,𝐻𝐴𝑍) and ultimate tensile strength (𝑓𝑢,𝐻𝐴𝑍) for heat-affected zones in alloy EN AW- 6082 T6 (EN1999-1-1, 2007).
𝑓0,𝐻𝐴𝑍 = 125 𝑁/𝑚𝑚2
𝑓𝑢,𝐻𝐴𝑍 = 185 𝑁/𝑚𝑚2
A method to experimentally achieve values for the heat-affected zone is proposed by Metusiak, as described by Wang. This consists of measuring Vickers hardness of heat-affected zone and using the relation showed in the following formulas, between Vickers hardness and yield and ultimate stresses (Matusiak, 1999, Wang, 2006).
𝑓0,2(𝑀𝑃𝑎) = 3,6𝐻𝑉 − 81 (1)
𝑓𝑢(𝑀𝑃𝑎) = 2,6𝐻𝑉 + 54 (2)
22 Where:
HV is the Vickers hardness
𝑓0,2(MPa) is the 0,2 % proof strength (MPa)
𝑓𝑢(MPa) is the ultimate tensile strength (MPa)
A different approach to achieve values from Vickers hardness was proposed by Myhr and Grong, as described by Đuričić. This approach gives lower values than the approach mentioned above (Đuričić et al., 2017).
𝑓0,2(𝑀𝑃𝑎) = 3𝐻𝑉 − 48,1 (3)
𝑓𝑢(𝑀𝑃𝑎) = 2,6𝐻𝑉 + 39,8 (4)
Đuričić et al. measured Vickers hardness in two different heat-affected zones. Vickers hardness is measured according to description in EN ISO 6507-1 (2005). Material within 20 mm of the weld is assigned HAZ1 and HAZ2 consist of material within 10 mm of HAZ1. Expression (3) and (4) are used to calculate 0,2 % proof stresses and ultimate strengths. The above results are presented in Table 6 (Đuričić et al., 2017).
Table 6: Stresses of material in HAZs (Heat affected zones) (Đuričić et al., 2017)
Zone HV 𝑓0,ℎ𝑎𝑧(MPa) 𝑓𝑢,ℎ𝑎𝑧(MPa)
HAZ 1 62 137,90 201,00
HAZ 2 75 176,90 234,80
2.2 Stress-strain relationship
Eurocode 9 part 1-1 (Annex E) describes the stress-strain relationship with piecewise linear models. Piecewise linear models are based on Hooke’s law for each of the lines representing the stress-strain relationship. Each line is represented with a different hardening modulus. These models will increase in accuracy as the number of lines is increased. This can be illustrated with a bi-linear model and a three-linear model. For the bi-linear model the following relationship can be assumed (EN1999-1-1, 2007).
23
𝜎 = 𝐸𝜀 for 0 < ε ≤ 𝜀𝑝 (5) 𝜎 = 𝑓𝑝+ 𝐸1(𝜀 − 𝜀𝑝) for 𝜀𝑝 < 𝜀 ≤ 𝜀𝑚𝑎𝑥 (6) 𝐸1 = 𝑓𝑚𝑎𝑥−𝑓𝑝
𝜀𝑚𝑎𝑥−𝜀𝑝 (7) Where:
𝑓𝑝 is the elastic limit of proportionality (Pa) 𝜀𝑝 is the strain corresponding to the stress 𝑓𝑝 𝑓𝑚𝑎𝑥 is the maximum stress of the material (Pa)
𝜀𝑚𝑎𝑥 is the strain corresponding to the stress 𝑓𝑚𝑎𝑥 𝐸 is the elastic modulus (Pa)
𝐸1 is the first hardening modulus (Pa)
For the three-linear model an additional stress-strain is added in the diagram and following relationships can be assumed (EN1999-1-1, 2007).
𝜎 = 𝐸𝜀 for 0 < ε ≤ 𝜀𝑝 (8) 𝜎 = 𝑓𝑝+ 𝐸1(𝜀 − 𝜀𝑝) for 𝜀𝑝 < 𝜀 ≤ 𝜀𝑒 (9) 𝜎 = 𝑓𝑒+ 𝐸2(𝜀 − 𝜀𝑒) for 𝜀𝑒 < 𝜀 ≤ 𝜀𝑚𝑎𝑥 (10) 𝐸1 = 𝑓𝑒−𝑓𝑝
𝜀𝑒−𝜀𝑝 (11) 𝐸2 = 𝑓𝑚𝑎𝑥−𝑓𝑒
𝜀𝑚𝑎𝑥−𝜀𝑒 (12) Where:
𝑓𝑒 is the limit of elasticity (Pa)
𝜀𝑒 is the strain corresponding to the stress 𝑓𝑒 𝐸2 is the second hardening modulus (Pa)
24
Figure 1: Bi-linear model (left) and three-linear model (right) of stress-strain relationship (EN1999-1-1, 2007)
From the 0,2 % proof strength, which is the conventional value for 𝑓0, the elastic limit of proportionality (𝑓𝑝) can be calculated with the formula (EN1999-1-1, 2007):
𝑓𝑝 = 𝑓0− 2√10𝑓0 if 𝑓0 > 160 𝑁/𝑚𝑚2 (13) 𝑓𝑝 = 𝑓0/2 if 𝑓0 ≤ 160 𝑁/𝑚𝑚2 (14) Where:
𝑓0 is the 0,2 % proof strength (Pa)
Calculating the axial stress (σ) of a specimen is done by dividing the axial load (P) by the cross- sectional area (A). If the initial area (A0) is used, the engineering stress is obtained. When a specimen is in tension the actual area of the cross-section is less than the initial area. By dividing the axial load on the tensioned area, a larger stress will be obtained. This is called true stress (Gere, 2004).
Engineering stress-strains can be converted into true stress-strains with the following approximations (Đuričić et al., 2017):
𝜀 = ln (1 + 𝜀𝑒𝑛𝑔) (15)
𝜎 = 𝜎𝑒𝑛𝑔(1 + 𝜀𝑒𝑛𝑔) (16)
Where:
𝜀𝑒𝑛𝑔 is the engineering strain 𝜎𝑒𝑛𝑔 is the engineering stress (Pa)
25 2.3 Design of K-joints
2.3.1 Failure modes
According to Eurocode 3, part 1-8, the failure modes that should be considered for hollow section joints, illustrated in Figure 2, are (EN1993-1-8, 2005):
a) Chord face failure, or chord plastification:
Plastic failure of chord face or of the chord cross-section b) Chord side wall failure:
Yielding, crushing or instability under the compression brace member, by crippling or buckling of the chord side wall.
c) Chord shear failure:
Shear failure in the chord d) Punching shear failure:
By crack initiation leading to rupture of the brace members from the chord member e) Brace failure:
Reduced effective width causing cracking in the welds or in the brace members f) Local buckling:
Buckling failure of a brace member or chord member at the joint location
26
Mode Axial loading Bending moment
a
b
c
d
e
f
Figure 2: Failure modes for jonts made of CHS-profiles (EN1993-1-8, 2005)
27
Figure 3: Gap K-joint with geometric sizes (EN1993-1-8, 2005)
Geometric sizes of a gap K-joint is given in Figure 3. If these sizes are in the range of validity given in Table 7, only chord face failure and punching shear needs to be considered (EN1993- 1-8, 2005).
Table 7: Validity range for welded joints between CHS brace members and CHS chords (EN1993-1-8, 2005)
0,2 ≤ 𝑑𝑖
𝑑0 ≤ 1,0 10 ≤𝑑0
𝑡0 ≤ 50 𝑑𝑖
𝑡𝑖 ≤ 50 𝑔 ≥ 𝑡1+ 𝑡2
Additional to validity range in Table 7 the angle of the brace members should be higher than 30˚ to ensure proper welds between chord and braces (Wardenier, 2001).
2.3.2 Design axial resistances for K-joints
Eurocode 3 part 1-8 suggests models for the calculations of axial resistances of brace members (𝑁1,𝑅𝑑, 𝑁2,𝑅𝑑) against chord face failure and punching shear failure in a K-joint (EN1993-1-8, 2005).
28 - Chord face failure
𝑁1,𝑅𝑑= 𝑘𝑔𝑘𝑝𝑓𝑦0𝑡0
2
𝑠𝑖𝑛𝜃1 (1,8 + 10,2𝑑1
𝑑0) /𝛾𝑀5 (17) 𝑁2,𝑅𝑑 =𝑠𝑖𝑛𝜃1
𝑠𝑖𝑛𝜃2𝑁1,𝑅𝑑 (18) Where:
𝑘𝑔 = 𝛾0,2(1 + 0,024𝛾1,2
1+exp(0,5𝑔
𝑡0 −1,33)) (19) 𝑁1,𝑅𝑑 is the resistance force in compressed brace member (N)
𝑁2,𝑅𝑑 is the resistance force in tensioned brace member (N) 𝑓𝑦0 is the yield strength of chord (Pa)
𝑡0 is the thickness of chord (m)
𝜃1 is the angle between compressed brace member and chord member (˚) 𝜃2 is the angle between tensioned brace member and chord member (˚) 𝑑1 is the diameter of compressed brace member (m)
𝑑0 is the diameter of chord member (m)
𝛾𝑀5 is the partial safety factor for resistance of joints in hollow section lattice girder, 𝛾𝑀5 = 1,0 (EN1999-1-1, 2007)
𝑘𝑔 is the joint geometry factor
𝛾 is the ratio of brace member to twice its wall thickness
g is the gap between brace members (m)
𝑘𝑝 is the chord stress factor, 𝑘𝑝 = 1,0 for k-joints without pre-loading (EN1993-1-8, 2005)
29 - Punching shear failure
𝑁𝑖,𝑅𝑑 = 𝑓𝑦0
√3𝑡0𝜋𝑑𝑖1+𝑠𝑖𝑛𝜃𝑖
2𝑠𝑖𝑛2𝜃𝑖/𝛾𝑀5 (20) Where:
𝑑𝑖 is the diameter of brace member i (m)
2.3.3 Aluminium softening reduction factor
In case of material characteristics not being affected by welding heat, resistance is higher than in the case of softening in heat affected zones. In case of completely softened joint there is a lower resistance than the experimental case. The aluminium softening for the design resistance is taken into account by introducing the aluminium softening reduction factor, kal (Đuričić et al., 2017).
𝑁1,𝑅𝑑,𝐴𝑙 = 𝑘𝑎𝑙𝑘𝑔𝑘𝑝𝑓𝑦0𝑡02
𝑠𝑖𝑛𝜃1 (1,8 + 10,2𝑑1
𝑑0) /𝛾𝑀5 (21) To determine 𝑘𝑎𝑙 the softening zone is defined with strength reduction factor, 𝜌0,ℎ𝑎𝑧, determined by the expression:
𝜌0,ℎ𝑎𝑧= 𝑓0,ℎ𝑎𝑧
𝑓0 (22) Where:
𝑓0,ℎ𝑎𝑧 is the yield strength for material in HAZ (Pa) 𝑓0 is the yield strength for material not in HAZ (Pa)
The size of the softening zone is called 𝑏𝐻𝐴𝑍. This varies for different types of thicknesses and welding techniques. For a TIG weld on a material with thickness between 0 and 6 mm, 𝑏𝐻𝐴𝑍 has a value of 30 mm. This length is set to be from the weld and 30 mm along the material (EN1999-1-1, 2007).
For a K-joint made from circular tubes, the cross section having the largest HAZ surface is considered. The total length of the softening zone L* is the circular arc of the chord that is in the softening zone. This consist of two parts, the arc length inside the brace member (l) and one part outside of the brace member with length 2𝑏𝐻𝐴𝑍. The total circumference of the chord is called L. The expression for 𝑘𝑎𝑙 in a K-joint made from CHS profiles is (Đuričić et al., 2017):
30 𝑘𝑎𝑙 = 1 −(1−𝜌0,ℎ𝑎𝑧)𝐿∗
𝐿 (23) Where:
𝜌0,ℎ𝑎𝑧 is the strength reduction factor for heat affected zone
𝐿∗ is the total softening zone arc length in the cross-section having the largest HAZ surface (m) L is the circumference of the chord member cross-section (m)
2.4 Previous analysis of k-joints
Deformation limit proposed by Lu et al. (1994)
According to Lu et al. as described by Choo et al. there are two limit strengths in a CHS joint, the ultimate strength, 𝑁𝑢, and the serviceability strength, 𝑁𝑠. A chord indentation of Δ𝑢 = 0,03𝑑0 corresponds to 𝑁𝑢, while 𝑁𝑠 corresponds to chord indentation of Δ𝑠 = 0,01𝑑0. If there is a peak in the load-deformation diagram, this deformation will be used as the ultimate deformation limit if it is lower than 0,03𝑑0. This study suggests that for CHS joints the ultimate deformation limit is the one governing the strength of the structure (Lu et al., 1994, Choo et al., 2003).
Research study of aluminium trusses by van Hove and Soetens (2016)
Van Hove and Soetens studied welded joints in a 30-meter span aluminium truss. Their truss consisted of K- and N-joints. This study investigated the possibility to apply design rules for steel, since there are no rules for aluminium design. The study consisted of a numerical analysis of the welded connections as well as a testing experiment to verify the numerical model. The material used in this analysis was aluminium alloy 6082 T6. They concluded that for both chord and brace sizes, the N-joints were governing. Further, the study concluded that failure mode and behaviour of aluminium joints are well predicted by the steel design rules. However, the failure load is overestimated by 8% for the truss that was investigated (van Hove and Soetens, 2016).
31
Experimental study of aluminium k-joints by Đuričić et al. (2017)
Đuričić et al. investigated three different k-joints made of aluminium alloy 6082 T6. This study consisted of a numerical analysis, experimental testing and hand calculations. Two different approaches for calculation of joint resistance was discussed in this study. One of them is to use the steel design rules found in EN1993-1-8, explained in chapter 2.3. The other approach is received from a previous study from Wardenier. The general expression for chord plastification for this approach is (Đuričić et al., 2017, Wardenier, 2001):
𝑁1 = 𝑓(𝛽)𝑓(𝛾)𝑓(𝑔′) 𝑓𝑦0∙𝑡0
2
sin(𝜃1)𝑓(𝑛′) (25)
Where:
𝑓(𝛽), 𝑓(𝛾) and 𝑓(𝑔′) are functions dependent on the joint members geometry
𝑓(𝑛′) is a function of the chord pre-load
𝑓𝑦0 is the chord yield stress (Pa) 𝑡0 is the thickness of the chord (m)
𝜃1 is the angle between chord and compressed brace member (˚)
Conclusion in this study is that with the use of aluminium softening reduction factor, 𝑘𝑎𝑙, explained in chapter 2.3.3, the analytical solution and the numerical and experimental analysis have a satisfactory match (Đuričić et al., 2017).
2.5 The finite element method
The principal of the finite element method is to divide a complex problem into several simpler problems and with the help of mathematics connect all the simple problems into an approximate solution of the original complex problem (Mac Donald, 2007). The logical diagram in Figure 4 presents the process of finite element analysis.
32
Figure 4: Logical diagram of the process of finite element analysis(Bathe, 2006)
Finite element analysis is introduced to examine physical problems that are too complex to examine just by using simple theoretical solutions. These problems include complex structures with many different cross-sections and loads, and structures with complicated geometry. To idealize the physical problem to a mathematical model some assumptions are required. These are made on the geometry, kinematics, materials, loading and boundary conditions. Then the mathematical model is formed, which is governed by differential equations. It is this mathematical model the finite element method solves. To solve this model, it is necessary to divide it into several smaller elements called finite elements. The size of the elements, known as mesh size, controls the accuracy of the solution. If the solution is not sufficiently accurate then it is necessary to repeat the numerical analysis with refined solution parameters, such as mesh size, until accuracy criteria are met. If the finite element solution is accurate then it converges to the exact solution as the number of elements is increased. Results from the analysis are interpreted and in case of insufficient accuracy, the aforementioned procedure is repeated (Bathe, 2006).
33 2.5.1 Boundary conditions and loading
It is important to consider which boundary and loading conditions must be used when building a model. The loads and constraints can be applied directly to the nodes. However, in solid modelling this can cause large stresses and local failure near the loaded or constrained nodes.
For solid modelling it is recommended to apply the loads and constraints to areas. This reduces the chance of local failure and the mathematical model is more realistic in relation to the real physical problem (Bathe, 2006).
2.5.2 Linear analysis
A linear analysis is performed when the material considered as linearly elastic, the displacements are infinitesimally small and the nature of the boundary conditions remain unchanged during the application of the loads on a finite element model. The equilibrium equations for a static analysis are:
𝑲𝑼 = 𝑹 (26)
Where:
K is the stiffness matrix (N/m) U is the displacement vector (m) R is the load vector (N)
These equations show a linear relation between load vector R and the displacement response U (Bathe, 2006).
2.5.3 Nonlinear analysis
When the assumptions in 2.5.2 are not used, a nonlinear analysis must be performed.
Nonlinear analyses can be categorized into different types based on which assumptions are used. These types are (Bathe, 2006):
- Materially nonlinearity only:
Infinitesimal displacements and strains with a nonlinear stress-strain relation - Large displacements, large rotations, but small strains:
34
Displacement and rotations of fibres are large, but extensions and angle changes between fibres are small, both linear and nonlinear stress-strain relations can be used.
- Large displacements, large rotations, and large strains:
Extensions and angle changes between fibres are large, both linear and nonlinear stress- strain relations can be used.
When performing a nonlinear analysis, it is important to consider which of the categories the physical problem is classified as. Even though the most general large strain formulation will give accurate results, it may be more efficient computationally to select a more restrictive formulation (Bathe, 2006).
2.6 ANSYS Mechanical APDL
ANSYS is a modelling package for solving mechanical problems with finite element method.
The mechanical problems include: static and dynamic structural analysis, heat transfer, fluid problems, acoustic problems and electro-magnetic problems. The static and dynamic structural analysis include both linear and non-linear analysis (ANSYS, version 18.2, Academic).
2.6.1 Element type used in ANSYS
For solid modelling in ANSYS with complicated geometry element type SOLID285 can be used. SOLID285 is a tetrahedral 4-node structural solid element. The element is defined by four nodes with four degrees of freedom each, translation in x, y and z direction and one hydrostatic pressure. The geometry of the SOLID285 element with node location and coordinate system is displayed in Figure 5. The element has plasticity, hyperelasticity, creep, stress stiffening, large deflection and large strain capabilities. Input data for the element includes isotropic, orthotropic and anisotropic material properties (ANSYS, version 18.2, Academic).
35
Figure 5: Geometry of SOLID285 element (ANSYS, version 18.2, Academic)
2.6.2 Element size and Meshing
When making elements in ANSYS the size of the elements must be taken into consideration.
To set element sizes there are different functions that can be used. The size of the element edge size can be set directly with the ESIZE function. A different function is to use SMRTSIZE.
With this function the software will create element sizes based on the geometry of the structure and the input size level. The size level is a number between 1 and 10 with 1 as the finest mesh and 10 as the coarsest mesh. There are also options of mapped or free meshing. Mapped meshing gives uniform elements through the whole structure but can be difficult to use in complicated geometries. Free meshing is not restricted to certain shapes and can be better to use for complex geometries. Meshing a structure is done by meshing functions LMESH, AMESH or VMESH based on which elements are present (ANSYS, version 18.2, Academic).
2.6.3 Multilinear isotropic hardening (TB,MISO)
Multilinear isotropic hardening is a model used for describing stress-strain relationships in ANSYS. The function TB,MISO creates a table with input of strain (ε), and stress (σ) corresponding to this strain using TBPT command. Materials assigned to these tables will follow the deformation curves of the assigned values (ANSYS, version 18.2, Academic).
36
3 Methodology
3.1 Introduction
The first part of the modelling process was dedicated to learning the software. This included reading and practicing on tutorials, starting with simple models and advancing to more complicated models. Parallel to this, different databases were researched and the experimental data in Đuričić et al. (2017) were selected for the verification of the numerical analysis. This was used as a base for all numerical modelling in this thesis. It was also investigated how to calculate design resistance in the different models and the approach from Eurocode 3, part 1-8 (2005) was selected. When all preparations were finished, the model that would be compared to experimental data was developed using computer software ANSYS 18.2. After this, models containing different parameters were constructed using the same input as the reference model, only changing one parameter at the time. Since a K-joint often has the same angle between both brace members and chord, it was decided to change both angles for the models. For modelling purposes, the weld was simplified. The braces were modelled as fixed to the chord member, without the fillet weld being modelled.
3.2 Different K-joints to be modelled
Table 8: Different models to investigate
Model number Chord profile Brace profile Angle (𝜽𝟏= 𝜽𝟐)
1 Ø50x2 mm Ø20x2 mm 45˚
2 Ø50x2 mm Ø20x2 mm 30˚
3 Ø50x2 mm Ø20x2 mm 60˚
4 Ø20x3 mm Ø20x2 mm 45˚
The experimental data from Đuričić et al. (2017) were used for model number 1. The members’
lengths were selected in order to avoid buckling of compressed brace member. In all models compressed brace member had length equal to 150 mm, tensioned brace member had length equal to 300 mm and chord had length equal to 750 mm. Since they were welded connections in aluminium under examination there was a need to consider the effect of the heat affected
37
zone. Data for two heat affected zones were obtained from the experimental analysis and implemented in the models. Geometry of the model is depicted in Figure 6.
Figure 6: Geometry of investigated models
3.3 Numerical analysis
3.3.1 Geometry
The geometry presented in chapter 3.2 was modelled in ANSYS with the help of simple solid cylinder functions. Split functions were used to make the curved shape of the braces at the intersection with the chord. The braces and chord were added together as a single volume to make them fixed, in order to simulate the weld. Symmetry conditions were applied to the structure, since stresses and deformations would be the same at both sides of the symmetry axis.
Initial geometry of the structure with brace angle of 45˚, as constructed in ANSYS, can be viewed in Figure 7.
38
Figure 7: Initial model of k-joint with angle of 45 degrees
3.3.2 Element selection and meshing
The structures have a solid geometry and the selection of finite elements is important. A large variety of elements in ANSYS were investigated and SOLID285 element type was selected.
SOLID285 has a tetrahedral shape which makes it optimal for structures with irregular shapes.
Elements with more nodes than SOLID285 can be found in ANSYS library. They offer some advantages over SOLID285 but since an academic version with node limitations is used, it was decided to apply SOLID285. To make models that will give a realistic solution it was decided to make a finer mesh in the vicinity of the connection and coarser mesh in the parts with a further distance to the connection. This was done by creating a different volume around the weld. All volumes within 100 mm of the centre of the connection were defined as a new volume.
Due to the complexity of the geometry of the K-joint, it was decided to use free meshing for the model. To select mesh sizes, the function SMRTSIZE was used. The volume furthest from the connection center was assigned a size level 10, and the volume closest to the connection was assigned size level 2. Each volume was meshed by itself using VMESH with the different size levels assigned. The resulting mesh responded well during the analysis. The meshed model is shown in Figure 8.
39
Figure 8: Mesh of k-joint
3.3.3 Material input
For all parts of the structure, the aluminium alloy EN AW-6082 T6 was used. Material properties was obtained from the experimental data in Đuričić et al. (2017). Value of elastic modulus was set as 69500 MPa and Poisson’s ratio was set as 0,33 for all materials.
- Chord and brace members
Đuričić et al. (2017) completed tests to investigate stress-strain relationship in the different CHS profiles. Among these tests, the chord profile and brace profile used in this thesis were investigated. The test showed engineering stresses for 0,2 % proof stress, 1 % tensile stress, 3
% tensile stress and ultimate tensile strength as well as ultimate elongation. Equation (15) and (16) are applied to calculate the true stresses shown in Table 9.
Table 9: True stresses in CHS profile
Profile(mm) 𝒇𝟎(𝑴𝑷𝒂) 𝒇𝟏%(𝑴𝑷𝒂) 𝒇𝟑%(𝑴𝑷𝒂) 𝒇𝒖(𝑴𝑷𝒂) Elongation (%)
Ø50x2 311,3 337,0 349,6 361,9 5,51
Ø20x2 274,0 286,3 297,8 321,6 5,52
40 - Heat affected zones
Đuričić et al. (2017) measured Vickers hardness in two zones of the heat-affected zone. One zone from weld and 20 mm along the material, and the second one from the edge of zone 1 and 10 mm along the material. The difference in hardness created two different engineering stress- strain relationships in the two zones. True stresses and strains are calculated from equation (15) and (16) Values for engineering and true stresses are showed in Table 10.
Table 10: Stresses for heat affected zones
Engineering stress True stress
Zone HV 𝒇𝟎,𝒆𝒏𝒈(MPa) 𝒇𝒖,𝒆𝒏𝒈(MPa) 𝒇𝟎,𝒕𝒓𝒖𝒆(MPa) 𝒇𝒖,𝒕𝒓𝒖𝒆(MPa)
HAZ1 62 137,9 201,0 138,4 211,9
HAZ2 75 176,9 234,8 177,7 247,5
All the models were assigned HAZ1 and HAZ2. This was done by creating three points on the weld, one at the right side of the brace, one at the left side of the brace and one at the middle.
All the elements within a distance of 20 mm from the points were assigned to HAZ1, and all the elements within a distance between 20 mm and 30 mm from the points were assigned to HAZ2.
3.3.4 Stress-strain curves
Values from 3.3.3 were assigned to different materials with multilinear isotropic hardening tables, which created deformation path curves. For chord and braces the points consisted of 0,2
% proof strength, 3 % tensile strength, ultimate tensile strength and the elastic limit of proportionality calculated from expression (13) and (14). For the heat affected zones 0,2 % proof strength, ultimate strength and elastic limit of proportionality were used.
Table 11: Multilinear isotropic hardening table for Ø50x2 mm in ANSYS
Point number
Strain (ε) Stress (σ) (MPa)
1 0,00287 199,74
2 0,00643 311,34
3 0,0296 349,60
4 0,0551 361,86
41
Figure 9: Plot of Ø50x2 mm stress-strain curve
Table 11 and Figure 9 presents the input multi linear isotropic table in ANSYS and the stress- strain diagram for CHS-profile Ø50x2 mm.
Table 12: Multilinear isotropic hardening table for Ø20x2 mm in ANSYS
Point number
Strain (ε) Stress (σ) (MPa)
1 0,00242 169,27
2 0,00592 273,95
3 0,0296 297,76
4 0,0552 321,64
Figure 10: Plot of Ø20x2 mm stress-strain curve
Table 12 and Figure 10 presents the input multi linear isotropic table in ANSYS and the stress- strain diagram for CHS-profile Ø20x2 mm.
42
Table 13: Multilinear isotropic hardening table for HAZ1 in ANSYS
Point number
Strain (ε) Stress (σ) (MPa)
1 0,000992 69,22
2 0,00398 138,45
3 0,0527 211,88
Figure 11: Plot of HAZ1 stress-strain curve
Table 13 and Figure 11 presents the input multi linear isotropic table in ANSYS and the stress- strain diagram for HAZ1.
Table 14: Multilinear isotropic hardening table for HAZ2 in ANSYS
Point number
Strain (ε) Stress (σ) (MPa)
1 0,00134 93,39
2 0,00454 177,70
3 0,0527 247,50
43
Figure 12: Plot of HAZ2 stress-strain curve
Table 14 and Figure 12 presents the input multi linear isotropic table in ANSYS and the stress- strain diagram for HAZ2
3.3.5 Boundary conditions and loads
Figure 13: Structure with applied boundary conditions and loading
The model was constrained in the same way as the experimental testing as shown in Figure 13.
One end of the chord was free while the end furthest from the connection was fixed and could not be displaced in any direction or rotation. The end of the tensioned brace was pinned so that it could not move in any direction, but it was free to rotate. The end of the compressed brace member was constrained so it could only move in the direction of the applied force. All areas at the symmetry axis were constrained with symmetry constraints. Constraints were applied on areas to avoid local failure around constrained parts of the model. Load was applied as pressure
44
at the top of the compressed brace and had different values for the models. Table 15 presents the pressure applied and the corresponding force.
Table 15: Pressure applied on compressed brace
Model Pressure (MPa) Force (kN)
1 147,47 16
2 176,83 20
3 132,63 15
4 212,20 24
3.3.6 Analysis type and postprocessing
Last step of modelling was to select analysis type static, turn on the large deformation analysis and set time steps. The time step was set to 0,05 which resulted in 20 iterations. The use of more iterations has been examined but the results obtained changed insignificantly so 20 iterations were chosen as a sufficient number. When the whole model was complete the solution process could be initiated. The solution time was about 5 minutes for each model.
The largest deformation was found where the compressed brace is in contact with chord face.
At this point there was measured deformation normal to the chord face. Deformation in the same direction was measured at two points 50 mm away from the point of maximal deformation. Average deformation of these two points was considered to be total shift at the point of maximal deformation and was subtracted from the maximal deformation, in that way only chord indentation was measured.
3.4 Interpretation of numerical results
After detailing and repeating numerical process, model 1 gave results that were comparable to the experimental data obtained from Đuričić et al. (2017). Force-deformation curves were developed from all models and ultimate strength and serviceability strength were obtained for the models with chord member thickness of 2 mm, according to chapter 2.4. For the model with chord thickness 3 mm, deformation above the limits set by Lu et al. (1994) was not obtained so the peak of the graph is selected as ultimate strength. Obtained strengths from the different
45
models was compared to each other to investigate how the change of angle and chord influenced the strength.
3.5 Hand calculations of K-joint
The calculation approach as described in chapter 2.3 was used. Hand calculations were done in two parts. First, where heat-affected zone was not taken into consideration, and secondly, where heat-affected zone was a part of the calculation.
3.5.1 Calculations without consideration of heat affected zone
In these calculations only yield strength of the chord material was used. Equation (17) was used to calculate design resistance in compressed brace member, 𝑁1,𝑅𝑑, against chord face plastification. Design resistance of tensioned brace member was the same, since 𝜃1 = 𝜃2. Punching shear resistance was also calculated with equation (20). Yield stress obtained from Đuričić et al. (2017) and from Eurocode 9 was used to calculate design resistance. Equation (19) was used to calculate 𝑘𝑔. 𝑘𝑝 = 1 for joints without chord pre-stress and 𝛾𝑀5= 1 is partial safety factor for resistance of joints in hollow section lattice girder. The calculations are shown in Table 16. Resistance for chord plastification has the index cp, resistance for punching shear is indexed ps and resistances with yield strength obtained from Eurocode 9 is indexed EN.
Table 16: Calculations according to Eurocode 3 part 1-8
Model 1 2 3 4
𝒌𝒈 1,657 1,657 1,668 1,529
𝒌𝒑 1 1 1 1
𝒇𝒚𝟎 (MPa) 311,34 311,24 311,34 311,34
𝒇𝒚𝟎,𝑬𝑵 (MPa) 250 250 250 250
𝒕0 (mm) 2 2 2 3
𝜽𝟏 (˚) 45 30 60 45
𝒅𝟏 (mm) 20 20 20 20
𝒅𝟎 (mm) 50 50 50 50
𝜸𝑴𝟓 1 1 1 1
𝑵𝟏,𝑹𝒅,𝒄𝒑 (kN) 17,2 24,2 14,0 35,5
𝑵𝟏,𝑹𝒅,𝒄𝒑,𝑬𝑵 (kN) 13,8 19,5 11,3 28,6
𝑵𝟏,𝑹𝒅,𝒑𝒔 (kN) 38,5 67,8 28,1 57,8
𝑵𝟏,𝑹𝒅,𝒑𝒔,𝑬𝑵 (kN) 31,0 54,4 22,6 46,4
46
3.5.2 Calculations with consideration of heat affected zone
Chapter 3.5.1 shows that the design resistance is the resistance related to chord plastification.
Further calculations are therefore only chord plastification resistance. In case of completely softened joint, EN1999-1-1 (2007) states yield resistance, 𝑓𝑦0,ℎ𝑎𝑧 = 0,5 ∗ 𝑓𝑦0. Since cross section is not completely softened this will give too low values for joint resistance. To calculate resistance of partially softened joint, equation (21) is used. For this aluminium softening coefficient, 𝑘𝑎𝑙, must be defined with equation (23). Calculations on 𝑘𝑎𝑙 are based on the cross- section of the chord with the largest amount of heat affected material. At this cross-section the arc length of the heat affected zone, L*, is the extent of zone, 𝑏𝐻𝐴𝑍, on both sides of the brace and the arc length within the brace member, 𝑙, illustrated in Figure 14.
Figure 14: Extent of heat affected zone(Đuričić et al., 2017)
Eurocode 9 gives 𝑏𝐻𝐴𝑍 to be 30 mm for TIG welding. Length within the brace member, 𝑙, is given by the angle 𝛼 = 2arcsin (𝑑1/2
𝑑0/2), where 𝑙 = 𝛼
360∗ 𝜋𝑑0. Total circumference of chord is 𝐿 = 𝜋𝑑0. To calculate 𝜌0,ℎ𝑎𝑧, equation (22) is applied. In the experimental data there are two different yield stresses in the heat affected zone while Eurocode 9 only describe one. For these calculations the average value of yield stress, 𝑓𝑦0,𝐻𝐴𝑍,𝑎𝑣, through the whole heat affected zone is used. Calculation of design resistances for fully softened cross-section (𝑁1,𝑅𝑑,𝐻𝐴𝑍, 𝑁1,𝑅𝑑,𝐻𝐴𝑍,𝐸𝑁) and for partially softened cross-section (𝑁1,𝑅𝑑,𝐴𝑙, 𝑁1,𝑅𝑑,𝐴𝑙,𝐸𝑁) are shown in Table 17.
